thread milling questions

[subi4ester]

today we were attempting to do some thread milling. First time for us and the results are not what we expected. Lookin to you guys to give some insight on whats going on or maybe thread milling should not be used in this material? Machine is a VF3/50, tool is kennametal tm25 parallel thread mill, using 14 tpi inserts, thru spindle coolant on, material is 8620 and clamped in vise rigidly, 15/16" thru hole, thread is 1"-14 to 1" depth, and using mastercam x4 for programming. Our issue is tool life, when we first started off, we were doing 2 passes to complete each hole ~800rpm, part turns out great but it sounded like the tool was not cuttin smoothly and assumin we are takin too much material each pass. Next we start increasing the number of passed and end up at 8 total per hole. sounds better but then inserts break. Next step slow down rpm ~400=broken inserts, increase rpm 1500 = broken inserts. try lowerin the number of passes, still breaking inserts, etc., etc. Basically we tried all kinds of shootin from the hip and broke the tool in the end. The completed threaded holes were all satisfactory, except a few during tool failure. We are using the feedrates vs. rpm that mastercam calculated.

Back to the ol ridgid tap, and cycle times are better as well. Where do we have it wrong? Any insight would be greatly appreciated. this is new to us.

thanks.

[makingchips]

Mastercam Feeds and speeds suck. It will cut, but tool life suffers. In 8020 I like to keep the chip load around .0015 per tooth .003 Max. Try 2300 RPM 8IPM at depth. This will use around 5Hp because of the .025 per flute at depth. In other words each tooth will be cutting at .0017 x 14 at depth= .024 full tool engagement. Don’t forget about a spring pass.

I personally like and have had great results with single profile thread mills.

Feed /rpm / number of flutes= chip load

Best of luck.

-MC

[christinandavid]

I trust you are climb-milling (thereby ramping up from the bottom of the hole).

DP

[78nova]

Some of this depends on the quality and use of the threads you need to form.

We are hobbing 15-5 stainless @ 36 RC. The thread is a 1.0"-12 UNF-3B, .540 minimum deep in a blind hole. We are using a .745 diameter spiral flute solid carbide OSG hob.

Each part has two holes and is done in 3 passes each. A rough pass, a finish pass and a spring pass. The rough pass is .005 undersize to the finish pass. The cycle takes the hob to the bottom of the hole and then ramps out. Running at 900 rpm @ 5.0 ipm. Coolant is Hangstefers Hard Cut 5418 Oil. Takes about 2 minutes to do 2 holes.

We hob a lot of threads but we also tap a lot of holes. For the most part, we tap our smaller threads up to 9/16" where we have the clearance in the bottom of the hole and we hob all of our larger threads and where we do not have clearance for the lead of a tap. The 15-5 stainless job we are using soild carbide, Scientific Cutting Tools spiral flute hobs to do a 5/16-24, 7/16-20 & a 5/8-18 thread. We get good life, form & depth that a tap would not. With these 3 holes we do not have the clearance you would need in the bottom of the hole for a bottom tap.

I have never used a thread hob with inserts but in your case it sounds like you may want to stick with rigid tapping the holes since it is working well for you. A spiral flute tap will work better also than a straight flute tap but if your holes are through holes it is not as important.

Insert thread hobs may very well have there uses but possibly the grade you used is not suited to your material.

What was the feedrate you used?

[Combat28Mech]

Try going to the carmex website. We've done some thread milling on our haas vf5 using their stuff and it seems to work quite well. We've done mostly bigger diameter holes we did a pipe thread for an intake manifold in aluminum and we also did some 1 1/2-12 threads in just some 1045. We've also got a 1/8-27 pipe thread we are in the process of doing and now we've got 3/4 and 3/8 that we will be working on. I would give that a try and see how it works for you. It writes the program for you on the website and their books actually give you a pretty good example on how to do it also. We didn't have any issue with speeds and feeds when we used it.

[offsetxyz]

I thread mill 3/4 16 in titanium at 1500 RPM and 1.5 IPM. Two passes one .010 off finish (.005 per side) and finish. It actually makes two roughing passes and 2 finishing, one 6 threads above the first. And always climb out of the hole. Never chipped and insert. ISCAR. They just put hair on the threads when they get dull. Is your minor diameter right. Is it an internal thread insert?